# wall function

 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 17, 2005, 08:00 wall function #1 Alex Guest   Posts: n/a Good Morning If I'm not wrong...in a boundary layer there is a region (viscous sub layer) where the velocity profile is linear and a region (log layer) where profile is logarithmic. If I take a look at the wall function formulation (solver theory pag 88), I can't see how it handle the linear profile. In other words: the logarithmic profile is used starting from the point at y+=11.06, but what about the linear profile that should be used in the viscous sub layer for y+<11.06 Thanks Alex

 May 17, 2005, 18:39 Re: wall function #2 Glenn Horrocks Guest   Posts: n/a Hi, The linear layer is extremely thin for most flows, so assuming the log layer starts at the wall is a good assumption for most flows. Glenn Horrocks

 May 17, 2005, 19:48 Re: wall function #3 Alex Guest   Posts: n/a Hi Glenn Really thanks for your umpteenth reply but I don't understand ! Are you saying that CFX 5.7 solver (sorry I didn't told you before ) assumes a log profile in the viscous sublayer ?? I found that in this region the velocity profile should be u+=y+ and the log-law start ( using the scalable wall function ) at y~*=max(y*,11.06). So it's my opinion that the log law start at y+=11.06 anyway and the profile is kept linear in the viscous sub-layer. What do you think?? Thanks and sorry if my questions are not interesting for the community. I'm just a student ! ! Alex

 May 18, 2005, 08:33 Re: wall function #4 Michael Bo Hansen Guest   Posts: n/a You can find more information at "CFX-5 Solver Modelling Turbulence Modelling" p. 119 where the low-Re method is described.

 May 18, 2005, 10:14 Re: wall function #5 Alex Guest   Posts: n/a Hi Michael I read again the pages. Maybe I understand but I need a confirmation for my idea. Starting from the wall, we assume a logarithmic profile untill the first node away from the wall.It has to be placed in the log layer at y+>11.06 (but if I use scalable wall function it isn't really a problem ). All the variables between the wall and the first node are calculated by the wall function. Further the first node, they are calculated by solving Navier-Stokes (RANS) equations. Am I rigth? Thanks Alex

 May 19, 2005, 00:48 Re: wall function #6 zxaar Guest   Posts: n/a i don't have cfx manuals so can't really comment about what cfx does, but as far as fluent is concerned, if the first point lies between plus < 11.06 and yplus > 3 (this 3 is not checked i have to check), but between these two bounds, fluent uses blending that is between both the values (log and linear),

 May 19, 2005, 04:54 Re: wall function #7 Alex Guest   Posts: n/a Hi Zxaar This behaviour is reasonable for me !! CFX doesn't tell anything about this Thanks

 May 19, 2005, 08:47 Re: wall function #8 Bak_Flow Guest   Posts: n/a Hi Alex, there is usually an elaborate explanation about wall functions, either in texts or in CFD manuals. However it is actually pretty simple. Every control volume, including those at the wall give the primitave variables (u,v,w,p...) by solving a momentum ballance (integral of advective and diffusive fluxes around the control volume). What the wall function does is gives you the wall shear stress! The scalable wall function just makes sure the calculation never uses a value below 11.06 for the yplus....then it crunches through to calculate the wall shear stress. Nice idea...assumes that the viscous sublayer is negligible or pushed into the wall. There are consequences to this of course if the viscous sublayer is important..maybe others? Regards, Bak_Flow

 May 19, 2005, 09:29 Re: wall function #9 Robin Guest   Posts: n/a Hi Alex, As Bak_Flow points out, the wall function is simply used to get the appropriate shear stress for the near wall control volume. If that control volume is far enough from the wall (i.e. Y+>11.06), AND the boundary layer is in equilibrium, the logarithmic profile assumption is reasonable. What the code does actually depends on the turbulence model you are using. The k-epsilon model can only use a logarithmic wall function. A potential problem with the standard wall functions can arise if the Y+ value drops below 11.06. In this case, the solution of the boundary layer away from the wall (beyond the first element) is dropping into the viscous sub-layer and the logarithmic profile assumption is no longer valid and despite having a finer mesh, your solution actually gets worse! CFX get's around this issue with k-e by using a so-called 'scalable' wall funtion. This caps Y+ at 11.06 and pushes the viscous sublayer into the wall. It's basically like assuming that your wall node is actually on the outer edge of the viscous sub layer, which isn't so bad, since that layer is very thin, but does introduce some degree of error, albeit less error than if you apply the standard wall functions. The advantage is that you no longer have to worry about having Y+ too small. That said, if the boundary layer is not in equilibrium, then the logarithmic wall function is still wrong and your need to resolve the viscous sub-layer. This is difficult to formulate with a k-e model, by quite straightforward with a k-omega type model. For k-omega type models, CFX will automatically blend between a linear and logarithmic profile within the boundary layer, if your spacing is fine enough. The SST model is a variant of k-omega which also accounts for the transport of shear stress and blends between a k-omega formulation near the wall, and a k-epsilon like formulation away from the wall. Note that other codes have SST, but the inventor of SST, Dr. Florian Menter, actually works for CFX and has continued it's development within CFX beyond what is in the common literature. So, to summarize, based on your concerns, I recommend running the SST model. Best regards, Robin

 May 19, 2005, 10:05 Re: wall function #10 Alex Guest   Posts: n/a This message is to really thank Bak_Flow and Robin. They gave me very interesting and meaningful explanations. Now it's all CLEAR !! Also I thank all the people that gave me a reply. Best regards Alex

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ivanyao OpenFOAM Running, Solving & CFD 1 October 12, 2012 09:31 AlmostSurelyRob OpenFOAM 3 June 24, 2011 13:06 johnblund OpenFOAM 0 March 10, 2011 09:50 yka8150 Main CFD Forum 0 September 21, 2009 23:08 Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00

All times are GMT -4. The time now is 15:00.